LTspice Quickstart Guide

Getting started with LTspice — installation, interface, command line, and first simulation.

About LTspice

LTspice is a general-purpose SPICE simulator with built-in schematic capture, developed by Analog Devices (originally Linear Technology). It is freely distributed without license or limits, with a large collection of component models for simulating analog circuits with high confidence.

Website: https://www.analog.com/ltspice
Training materials: https://www.analog.com/ltspice (videos, articles, tips)
Change log: Help > Show LTspice Change Log

Installation

Download: https://www.analog.com/ltspice

Updates:

Program: Help > Check for LTspice updates
Components/models: Tools > Update components

Important: Files in %LOCALAPPDATA%/LTspice are replaced on update. Do not place or edit files in this directory. To add custom symbols or simulation files, place them in the user files directory (default Documents\LTspice\), or in directories listed under Settings > Search Paths (symbol search paths for symbols, simulation library search paths for model/subcircuit files).

Basic Workflow

Draw a circuit (or open an example: File > Open Examples…)
Place simulation command (.tran, .ac, etc.) as text on schematic
Run simulation (Run button or default shortcut Alt+R)
Click nodes on schematic to plot voltages; click components to plot currents
Iterate the circuit until desired behavior is achieved

File Types

Extension	Description
`.asc`	Schematic file (graphical circuit)
`.net`, `.cir`, `.sp`	SPICE netlist (text circuit description)
`.raw`	Simulation output waveform data
`.log`	Simulation log (errors, measurements, operating point)

A schematic is converted to a netlist (.net) automatically when simulated. You can also open and simulate text netlists directly.

Editing Modes

Assisted Mode — Specialized Component Editors

Right-click on the body of a component to open its specialized editor. Works for: resistors, capacitors, inductors, diodes, BJTs, MOSFETs, JFETs, voltage/current sources, and hierarchical blocks. These editors provide access to component databases.

Expert Mode — Edit Visible Attributes

Point at a visible attribute (value, name) and right-click. The cursor changes to a text caret, allowing direct editing. Convenient for quickly changing component values.

Super Expert Mode — Full Attribute Editor

Hold Ctrl and right-click on the component body. Opens a dialog showing ALL available symbol attributes with visibility checkboxes.

The toolbar provides one-click access to common commands. Toolbar visibility can be toggled from View > Toolbar, and the icon style/size is configurable under Tools > Settings (see Settings).

Icon	Button Name	Keyboard Shortcut
	Settings
	New Schematic	Ctrl+N
	Open	Ctrl+O
	Save	Ctrl+S
	Print	Ctrl+P
	Configure Analysis	A
	Run/Pause	Alt+R
	Stop	Alt+S
	Tile Windows Vertically
	Tile Windows Horizontally
	Cascade Windows
	Zoom Area	Z
	Zoom Back	Shift+Z
	Zoom to Fit	Space
	Autorange	Ctrl+Y
	Pick Visible Traces
	Wire	W
	Ground	G
	Voltage Source	V
	Resistor	R
	Capacitor	C
	Inductor	L
	Diode	D
	Component	P
	Label Net	N
	Text	T
	SPICE Directive	.
	Delete Mode	Backspace or Delete
	Duplicate Mode	Ctrl+C
	Move Mode	M
	Stretch Mode	S
	Rotate	Ctrl+R
	Mirror	Ctrl+E
	Undo	Ctrl+Z
	Redo	Ctrl+Shift+Z
	Search	Ctrl+F

Keyboard Shortcuts

View shortcuts: Help > Keyboard Shortcut Cheat Sheet (always-on-top window)
Customize: Click Edit Keyboard Shortcuts button in cheat sheet
Save/load shortcut sets from files
Shortcuts persist between sessions

See LTSPICE-KEYBOARD-SHORTCUTS.md for the full shortcut reference.

Command Line Switches

Executable path (depends on installation method):

Per-user install: C:\Users\<username>\AppData\Local\Programs\ADI\LTspice\LTspice.exe
System-wide install: C:\Program Files\ADI\LTspice\LTspice.exe

LTspice.exe [options] [filename]

Switch	Description
`-b`	Batch mode (e.g., `ltspice.exe -b deck.cir`)
`-Run`	Open and immediately simulate
`-netlist`	Convert schematic to netlist (batch)
`-PCBnetlist`	Convert schematic to PCB netlist (batch)
`-big` / `-max`	Start maximized
`-alt`	Use alternate solver
`-norm`	Use normal solver
`-ascii`	ASCII .raw files (degrades performance)
`-FastAccess`	Convert .raw to Fast Access format
`-encrypt`	Encrypt a model library
`-ini <path>`	Specify alternate .ini file
`-I<path>`	Add symbol/file search path
`-sync`	Update component libraries
`-version`	Print version
`-FixUpSchematicFonts`	Fix old schematic font sizes
`-FixUpSymbolFonts`	Fix old symbol font sizes

Environment variables:

PASTE_OMEGA — paste Unicode Ω instead of “Ohm”
CAPITAL_KILO — prefer uppercase for multipliers > 1

Example Circuits

Access via File > Open Examples…

Directory	Content
`Educational/`	Non-commercial examples illustrating analysis types and features
`Applications/`	Example circuits for ADI products (verify component values for your design)

Location on disk: %LOCALAPPDATA%\LTspice\examples\

LTspice includes Windows Explorer preview handlers for .asc files.

Settings

Access via Tools > Settings. Items marked with * persist between sessions.

Setting	Description
Marching Waveforms	Incrementally plot during simulation
Generate Expanded Listing	Dump flat netlist to log file
Save all open files on start	Sync in-memory and disk schematics
Automatically delete .raw files	Clean up waveform data on close
Background image	Custom JPEG at `%USERPROFILE%\LTspice.jpg`
Toolbar Style	New (2026) or legacy icons
Toolbar icon size	Larger or smaller icons
RAM for Fast Access	Tune memory for file conversion
Directory for Temporary Files	Location for update downloads

First Simulation — RC Low-Pass Filter

As Schematic

File > New Schematic
Place components: voltage source, resistor, capacitor, ground
Wire them together
Set values: V1 = PULSE(0 1 0 1n 1n 0.5u 1u), R1 = 1K, C1 = 100n
Add simulation command as text: .tran 5u
Click Run
Click the output node to see the waveform

As Netlist

Create a file rc_filter.cir:

* RC Low-Pass Filter
V1 in 0 PULSE(0 1 0 1n 1n 0.5u 1u)
R1 in out 1K
C1 out 0 100n
.tran 5u
.end

Run from command line:

ltspice.exe -b "C:\path\to\rc_filter.cir"

Or open in LTspice and press Run.

Critical Conventions

Unit Notation

Always use u for micro (1e-6), never the μ symbol in netlists.

C1 out 0 1u        ; correct: 1 microfarad
.tran 100u          ; correct: 100 microseconds

See SPICE-SYNTAX-REFERENCE.md for the full multiplier table.

Common Pitfall

1M = 1 milli (1e-3), not 1 mega. Use 1Meg for megaohms.

File Paths

Always use complete absolute paths when opening files from command line:

ltspice.exe "C:\Projects\MyCircuit\filter.asc"